# How to create NPT (national pipe taper) threads using inventor

I have had people ask me on here how I model npt threads for some of the parts I make, so I figured I would put it out there for others to see as well. Note: if you look at the threaded models I have on this website you will see that I have clearly taken more time on some of them than others, this tutorial will teach you how to do it the right and proper way.

1. ### Step 1:

Note: I tagged this as intermediate but only because there are several steps, once you get the hang of it this isn't hard and I will walk you through this one little bit at a time. Lets say we want to model a fitting of some kind that has 1" NPT threads, we could just use the "thread" tool that inventor comes with, but it doesn't truly model threads it just overlays an image on your part that kinda looks like threads and in a drawing can be called out as such. If we want to make it right we need to actually model them as they would be on a real physical part, that means the first thing we need to do is determine if the threads are male or female (male means the threads are on the outside, female means the threads are on the inside) I will teach you how to do it both ways.

2. ### Step 2:

Lets say I want to make a camlock adaptor (if you dont know what that is dont worry about it this technique can be applied to anything) Note: I'm not actually measuring this part I'm just making something that looks close for demonstration purposes.

3. ### Step 3:

Lets say that we know how to model everything else except the threaded part, if you dont know how to model the rest of it dont worry about it, you make threads the same way for any kind of part. I said the first step was to determine whether the threads you are trying to model have male threads of female threads, this one clearly has male threads so we will start there.

The second thing to determine is what size threads your part has. NPT pipe sizes can be confusing since the dimension it is called has very little to do with its actual dimensions. In step (1) I just stated that we will be making 1" NPT threads, if we look up "NPT dimensions" on the internet we find that all 1" NPT pipes, fittings and anything else have an actual O.D. (outside diameter) of 1.32". The I.D. (inside diameter) varies with pipe schedule, so once you know what schedule you have you can look up the I.D. by searching the internet for "schedule ** dimensions" (where ** is the pipe schedule you are working with). Once you know the O.D. and I.D. of your part we can begin making threads.

4. ### Step 4:

The first thing we need to do is create an accurate profile to cut the threads into. We know from the previous step that NPT connections all have a specific O.D. but they dont maintain that I.D. through the whole length of the threaded section, the "T" in NPT stands for 'Taper' which means NPT threads are on an angle. 3.576 degrees to be exact. The taper is defined as 1/16" of drop in radius for every 1" of thread length. What I do to make this simple is I define my vertical drop as (horizontal length/16).

If you dont have a part in front of you to measure its a good bet that the length of your threaded section is going to be just slightly longer than the maximum thread engagement for your pipe size. (this information can be found by searching the internet for "NPT thread engagement")

Note: because we're going to revolve this profile, the vertical dimensions are radii and thus exactly half of the O.D.

5. ### Step 5:

Next we are going to do a full revolve of our profile we just drew, something I didn't mention is that it is good practice to orient sketches on the origin that way you can revolve around established axes. When you are done youre part should look like the picture.

6. ### Step 6:

Thuis next step seems little but it is important for creating realistic threads, put a small chamfer around the outside edge of your threaded profile. make the chamfer 45 degrees and about 1/3 to 1/2 the thickness. (this could be built into the profile but doing it this way is less complicated.

7. ### Step 7:

Now its time to make the threads. Create a sketch on the same plane you created the revolved profile on, and draw the shape that matches the space between your threads. If you want to be 100% exact you can look this information up but I find that a 1/16" x 1/32" x 1/64" trapazoid seems to work well for most applications. For bigger thread sizes you may want to make the trapazoid larger.

Either way make sure your shape protrudes down into the revolved profile you created in the previous steps, use the "project geometry" tool to project the tapered line from the profile onto your currecnt sketch and constrain the top edge of your trapazoid (or whatever shape you are using) to be colinear with that tapered line. Make sure the trapazoid is close to the beginning of the taper but not on it.

8. ### Step 8:

We are going to use this little trapazoid to cut a helical path through the bulk material by using the "coil" feature. First of all make sure that your trapazoid shape is selected as the "profile" and then select the appropriate axis. there is an option withing the coil feature window to select the "axis" direction, make sure it is going the right way. Next set the function to 'cut' (the second button from the top on 2013 version) and make sure the coild direction is correct. (most threads in the world are right hand threads, meaning as it rotates clockwise it travels away from you).

On the "coil size" tab within the coil feature window select "revolution and hieght" as the type and then input a hight that goes slightly beyond the tapered section you are trying to thread, for "taper" enter 3.577 (if you try to enter exactly 3.576 it wont work) then select the appropriate amount of revolutions. you can find out how many revolutions per inch your thread has by searching the internet, though this number often has to be modified slightly to appear correct in pictures.